IABU-UNIT99-LA04-Thermal Abaqus Documentation

thermal Abaqus

1. Appendix content: Introduction Steady-State Heat Transfer Transient Heat Transfer Thermal Interfaces Thermal-Stress Analysis Appendix 4 : Heat Transfer and Thermal-Stress Analysis 2 hours

2. Introduction (1/4) Heat transfer analysis is appropriate when: There is a need to obtain the temperature field in a solid or fluid. Temperature is not influenced by other unknown fields All three modes of heat transfer may be present in an Abaqus analysis. q 2

3. Introduction (2/4) The uncoupled heat transfer analysis capability is available only with Abaqus/Standard. Transient analysis Obtain history of the response over time with heat capacity and latent heat effects included. Steady-state analysis Obtain long-term solution under given set of loads and boundary conditions. The coupled thermal-mechanical analysis capability is available in both Abaqus/Standard and Abaqus/Explicit. Abaqus/Standard: transient (quasi-static) and steady state analysis capability Abaqus/Explicit: transient (dynamic) analysis capability only.

4. Introduction (3/4) Nonlinearity Either type of analysis can be nonlinear. Sources of nonlinearity include: Temperature dependence of material properties: k (  ). Nonlinear surface conditions: Radiation: q (  ) = f (  4 ). Temperature-dependent film coefficients: h (  ). Loads that vary nonlinearly with temperature. Latent heat (phase change) effects In Abaqus/Standard user subroutines ease definition of nonlinear effects : FILM Describe convection conditions: h ( q , x ). DFLUX Describe distributed loadings: q ( q , x ). HETVAL Describe internal heat generation as a function of solution-dependent state variables: r ( SDV ).

5. Introduction (4/4) Temperature scale conversion Allows the use of any temperature scale. The conversion to absolute temperature, whenever needed, is done internally by Abaqus. Element selection Abaqus offers heat transfer elements as well as coupled thermal-mechanical elements . Pure diffusion (i.e., heat transfer) elements are available only with Abaqus/Standard. First- and second-order elements are available. Use second-order elements for smooth diffusion and conduction. Use first-order elements for highly nonlinear, discontinuous conduction such as phase changes (latent heat effects). Thermally-coupled elements use a first-order interpolation for the thermal response (the displacement field interpolation may be first- or second-order.)

6. Steady-State Heat Transfer (1/6) Example: Two-dimensional heat transfer with convection Reference : Abaqus Benchmark Problem 4.3.4 (modified) Conductivity = 52 W/m/ º C Film coefficient = 750 W/m 2 / º C Boundary conditions: q = 100 º C along AB Heat flux = along DA Convection to ambient temperature at º C along BC and CD Objective: Find q at E Target solution: 18.3 º C at E

7. Steady-State Heat Transfer (2/6) Thermal material properties and element selection Only thermal conductivity is required for a steady-state heat transfer analysis. First-order interpolation of the temperature field

8. Steady-State Heat Transfer (3/6) Procedure definition: Steady-state heat transfer Incrementation data for a steady-state heat transfer analysis is similar to that for a static analysis .

9. Steady-State Heat Transfer (4/6) Boundary conditions: Prescribed temperatures on the bottom of the plate bottom

10. Steady-State Heat Transfer (5/6) Film conditions: Interactions with the ambient on the top and side of the plate side top h q amb

11. Steady-State Heat Transfer (6/6) Results Steady-state temperature distribution Nodal temperature at target location obtained by probing contour plot values Target solution is 18.3ºC

12. Transient Heat Transfer (1/9) Example: Two-dimensional heat transfer with convection Conductivity = 52 W/m/ º C Specific heat = 434 J/kg/ º C Density = 7832 kg/m 3 Film coefficient = 750 W/m 2 / º C Boundary conditions: q = 100 º C along AB Heat flux = along DA Convection to ambient temperature at º C along BC and CD Objective: Find q at E Target solution: 18.3 º C at E at steady state

13. Transient Heat Transfer (2/9) Changes to material definition Additional material properties required for transient thermal analysis Constant pressure specific heat is required for thermal flow problems (CFD)

14. Transient Heat Transfer (3/9) Changes to procedure definition: Transient heat transfer Controls automatic time incrementation: max D q = 30 in any increment . Time incrementation data similar to that for dynamic structural analysis Analysis stops if steady-state conditions are reached ( q < 0.0005 ) .

15. Transient Heat Transfer (4/9) Initial conditions; changes to boundary and film conditions Initial temperatures are predefined as fields in the Initial step (only required if initial temperature not equal to zero). Boundary and film conditions are applied instantaneously (default).

16. Transient Heat Transfer (5/9) Results Steady-state temperature distribution Transient simulation: Comparison of transient and steady-state results at selected node Transient temperature history Steady-state temperature

17. Transient Heat Transfer (6/9) Abaqus/Standard: Minimum usable time increment In implicit transient heat transfer analysis there is a minimum usable increment size — the mesh refinement determines the smallest usable time increment. A simple formula provides the minimum usable increment. Abaqus/Standard does not enforce this minimum usable increment size . This minimum is a requirement only for second-order elements, but it is recommended for all heat transfer elements.   D l is the distance between nodes for element near surface with highest temperature gradient

18. Transient Heat Transfer (7/9) What happens if you violate this formula? Consider the following one-dimensional case: Conductivity = 52 W/m/ º C Specific heat = 434 J/kg/ º C Density = 7832 kg/m 3 Initial conditions: q = º C everywhere Boundary conditions applied at time : q = 100 º C at point A q = º C at point B Objective: Find q ( t ) along AB  

19. Transient Heat Transfer (8/9) Time Too small!

20. Transient Heat Transfer (9/9) Avoiding minimum usable time increment Symptoms of time increments being too small: Spurious oscillations in the temperature. The temperature increases when it should decrease. The temperature decreases when it should increase. Resolution : Use larger time increments (do not accept early transient solution) or Refine mesh near surface

21. Thermal Interfaces (1/2) Thermal interface modeling Capability allows modeling of heat transfer across thin interfaces. Low thermal conductivity. Large temperature differences across interface. In Abaqus these effects are modeled using surface-based interactions (similar to contact). Surfaces are in close proximity but have distinct properties on either side of the interface. Available thermal interactions include: Heat conduction between surfaces. Radiation between closely-spaced surfaces. Frictional heat generation (fully coupled thermal-stress analysis only ).

22. Thermal Interfaces (2/2) Cavity radiation (Abaqus/Standard only) Cavities are made up of radiating surfaces. Surfaces are defined as a set of individual facets using the same syntax as contact surfaces. Surface emissivity can be temperature dependent. Viewfactors are calculated automatically in two-dimensional, three-dimensional, and axisymmetric geometries. General shadowing, blocking, and symmetry capabilities. Surface motions: Option to prescribe displacements and rigid body rotations during a heat transfer simulation. Automatic recalculation of viewfactors during the motion.

23. Thermal-Stress Analysis (1/9) Sequentially coupled problems Thermal field affects the mechanical field. Mechanical properties change with temperature. Thermal expansion. Mechanical field does not affect the thermal field. Two jobs required to solve thermal stress problem Thermal and mechanical fields solved in sequence (thermal followed by mechanical)

24. Thermal-Stress Analysis (2/9) Fully coupled problems Thermal field affects the mechanical field as above. Mechanical field affects the thermal field. Mechanically generated heat-due to plastic work or friction. Deformation can change conduction, radiation, etc. One job required (thermal and mechanical fields solved simultaneously)

25. Thermal-Stress Analysis (3/9) Sequentially coupled example Plane stress Mechanical material properties: E = 206.8 GPa n = 0.3 Yield stress = 248.2 MPa a = 7.5 x 10 - 6 Loads and boundary conditions: Clamped along AB Symmetry along DA q ( t ) from transient response applied as “loads” Objective: Find mechanical response due to temperature

26. Thermal-Stress Analysis (4/9) Procedure definition: General static analysis Time period chosen to correspond to that of the thermal analysis This is not required: Abaqus will scale thermal time period to the mechanical one if necessary.

27. Thermal-Stress Analysis (5/9) Applying temperatures in a sequential thermal-stress analysis Temperatures can be applied directly, read from a file, or prescribed in a user subroutine. In sequentially coupled problems temperatures are usually applied by reading the output database or the results file from the corresponding heat transfer analysis. Mismatched meshes are permitted.

28. Thermal-Stress Analysis (6/9) Initial temperatures are read in from heat transfer analysis Heat transfer analysis results are read in as a predefined field Data specifies what portion of the thermal analysis drives the mechanical analysis First-order elements can be used in the heat transfer analysis, and second-order elements can be used in the thermal-stress analysis. Abaqus will use temperatures at the corner nodes in the thermal-stress simulation to calculate the temperature at the stress/displacement element’s midside nodes.

29. Thermal-Stress Analysis (7/9) Performing a sequential thermal-stress analysis using Abaqus/Explicit Two options available: Run a heat transfer job in Abaqus/Standard followed by an Abaqus/Explicit job Pass temperatures to the Abaqus/Explicit job via the output database or results file Advantage: Second-order heat transfer elements available Disadvantage: 2 jobs required Adjust the properties in the fully coupled procedure in Abaqus/Explicit to execute a sequential analysis within the same job The idea is to stem the flow of information in the mechanical → thermal direction (thermal analysis is uncoupled from the structural analysis). Advantage: Only 1 job is required Disadvantage: limited to element library in Abaqus/Explicit .

30. Thermal-Stress Analysis (8/9) For option 2: Set the fraction of plastic dissipation converted into heat to zero. Equal to 0.9 by default; setting it to zero uncouples the thermal response from the mechanical response (in the absence of frictional work). Mechanical response still coupled to thermal response via material properties and thermal expansion. Use mass scaling for an efficient analysis. Scaling factor equal to 1.0e+10 .

31. Thermal-Stress Analysis (9/9) Results Mises stress distribution at steady-state temperatures (Abaqus/Standard analysis) Mises stress distribution at steady-state temperatures (Abaqus/Explicit analysis) Abaqus and Isight can be combined to automate sequential thermal-stress simulation

32. Portfolio Connections: Isight Abaqus and Isight can be combined to automate sequential thermal-stress simulation. Example: Integrating Isight with the Abaqus Welding Interface (AWI ) Simple DOE workflow running a test AWI model. Input parameter : Torch Application time Output parameter : Max misses stress in the whole model Many of the operations in the AWI could be automated, including bead selection for pass etc. Doing so has the potential to develop a more complete Design Exploration of Weld Mechanics For more detail see SIMULIA Learning Community post #28366 : Isight Corner: How to Integrate Abaqus Welding Interface (AWI) with Isight? ( https://swym.3ds.com/# post:28366 ) Power of the Portfolio